Creating cuts across sheet metal bends

Have you tried all the buttons in SOLIDWORKS?

I don’t blame you if you haven’t.

I would be surprised if you had, actually.

There are just so many of them. There are complete toolbars full of useful features that I have never even touched (Wait, there is a Web toolbar? Ok bad example).

Unfold sheet metal body

If you do machine or prototype design, chance is you use the sheet metal toolbox a lot. I now have the feature just for you. Say you want to create this simple bracket. Drawing the flat pattern on a piece of paper is easy. When you don’t know the proper techniques, creating it using the computer could take a while.

Simple bracket with a cut across a bend

The cut that goes across the bend is the topic of interest here. How can we add that one, quickly and properly dimensioned with regard to the other features? You could create it by adding an extruded cut, followed by a few fillets. But the shape really is just a slot, so sketching that would be the preferred way. Let’s recreate this part.

The outline is the first step. Forget drawing a square and adding two flanges, this is faster and awesomer.

Outline sketch

Step 2: Creating a base flange. I’ve used a bend radius that matches the sheet thickness as a general rule of thumb.

Extrude base flange from midplane

The K-factor is used to calculate how much material is required to make the bends. The upper limit is 0.5 because it is defined as the ratio of the neutral line position divided by the sheet metal thickness. For this radius of 1 times the material thickness, a factor of 0.4-0.45 would actually be more accurate. It all depends on the machine and material parameters.

Unfolding

Now for the main event:

Unfolding bends

The unfold feature is the one that you need. Click it, select a face that should remain fixed and click the button to collect all bends. I deleted one of the bends from this list to unfold only one bend.

Note that this unfold/fold feature is not the same as the flat pattern. The flat pattern is a special configuration for sheet metal parts that has all bends suppressed. With the unfold feature, you can selectively unfold single bends.

You can see the result of the unbending in the image below. You can now properly create a sketch and dimension the slots with regard to the sides.

Adding the slot sketch. If you’re wondering how to add the 50mm dimension, hold shift and click the arc 🙂

Now all you need to do is extrude the cut, fold it back by adding a fold feature and there it is:

Feature tree

Every unbend and bend you add is a new feature, therefore you can suppress them like any other feature. You can see the feature tree in the following image:

Feature tree including unbend and bend features

Caveats

As always, patterns might not always work in combination with this feature. I’ve seen weird cases where the pattern suddenly stopped working. Usually, a workaround is recreating the seed feature and the pattern. Fortunately, I got it to work flawlessly this time.

A linear pattern can be folded back as well (usually)

Performance

The official SOLIDWORKS documentation remarks that one should only flatten the bends that are required. Flattening all bends every time will naturally result in a lower performance.

Summary

This feature lets you create single extrude cuts by temporarily unfolding sheet metal bends. Rather than the flat pattern view (which should not be unsuppressed before adding a feature), this allows you to actually add complex cuts using simple sketches. As a result, you once again have all the design freedom that the laser cutter once gave you.